Drill Cycle on HAAS ignoring Fusion

[ICanSpinIt]

Under the drill op I have the minimum and reduction pecking cycle (full retract) set to 0.05" 

The post processor outputs the cycle as N105 G98 G83 X1.2205 Y0. Z-1.65 R0.1 Q0.13 P0 F5. 

Even after manually changing the reduction to R0.05 the machine still ignores and drills to somewhere around .2" 

There are suppose to be 30 pecks but am only getting 13

Machine= Haas tm-2 (early 90's)

What is going on?

[johnswetz1982]

R is the clearance plane. Q is the Peck depth

https://www.haascnc.com/service/codes-settings.type=gcode.machine=mill.value=G83.html 

[ICanSpinIt]

Thank you for the correction! Do you know why fusion won't export the drill cycle as a J? or is this a post processor issue?

[johnswetz1982]

Can you attach your file by File>Export>*.f3d and attch to thread?

[engineguy]

@ICanSpinIt 

Here is the code for a G83 peck drill cycle using the HAAS Pre NGC Control Post Processor and it appears to be correct.

I used your 0.05in value with a 0.1in retract as that is what is in your line of code that you posted.

The total number of pecks is actually 34 which is the first peck plus the number of pecks @ 0.05in in a distance of 1.65in, simple math shows that would be 33 pecks, therefore total is 34 pecks. Code is below!!

%
O05959 (MAIN SPINDLE, UPPER TURRET)
(Using high feed G1 F500. instead of G0.)
(T1 D=0.5 CR=0. - ZMIN=-1.65 - drill)
N10 G90 G94 G17
N15 G20
N20 G53 G0 Z0.

(Drill2)
N25 T1 M6
N30 S2000 M3
N35 G54
N40 M8
N45 G0 X-0.0000 Y0.0000
N50 G43 Z0.6 H1
N55 G0 Z0.1
N60 G98 G83 X-0.0000 Y0.0000 Z-1.65 R0.1 Q0.05 F5.
N65 G80
N70 G0 Z0.6

N75 M5
N80 M9
N85 G53 G0 Z0.
N90 X0.
N95 G53 Y0.
N100 M30

%

Regards

Rob

[ICanSpinIt · Accepted solution]

The post processor wasn't setup to accept drill PECK cycles. Corrected post and now machine exports the I,J,K commands.